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I've been having an issue since installing Creo 2.0 where I'm trying to create an assembly and pull in parts, but they're not constraining correctly. I was watching a Creo Primer video, and the speaker said that Creo is smart and will automatically learn the constraints you've been using on a part and will apply them the next time you pull the part in. My problem is that mine will not automatically learn the constraints, and I have to go back and re-select the parts and constrain them manually. This isn't a terrible issue, but it is annoying when the video says that something SHOULD happen and it doesn't. The first file that I put in for the assembly file was the cube and then started adding cubes and shafts (cube file isn't labeled as cube currently).
Solved! Go to Solution.
I think those videos are half educational and the other half propaganda. There is such a thing as Component Interfaces, but I don't know anything about "automatic". I don't use these so I am not sure what the video might be referring to.
You wouldn't know anything about creating threads, would you?
Sure, care to start a new thread?
No pun intended?
D'OH! I missed that one
I created the thread. It's called 'Creating threads?'
is your config option 'create_temp_interfaces' set to yes?
Nice find, Charlotte. Why would that be "no" by default?
Antonius, would you expect this to be a default ? This will result user in entering with-interface type placement by default if there is at least one similar compoinent already assembled somewhere, not having explicit interface created anywhere ... on the other hand this is clear automation.
Oooohhhh... Hmmmm... that always makes it a touch choice as to whether I want to remember an option or add it to the config.pro file.
Ideally, the UI would be friendly about giving you the choice. Either with prompts or a checkbox dialog like "would you like to re-use these constraints in this session?".
How do I check this?
File > Options > Configuration Editor
It was set to 'no'. I had to tell it to show all options and then was able to find the setting. That setting seems to have fixed the issue. Thanks!!
I'm having this issue as well. Just switched to Creo 2.0 from WF5, and immediately noticed that I have to go and reconstrain a repeated part every single time I place it. In WF5, the references window would retain the part features that were selected before, and you would only have to select the corresponding features of the assembly to constrain to. Needless to say, my productivity in asm mode has gone down as a result. Hoping soemone comes up with the answer, and thanks to Christopher West for starting the thread!
This brings up the question:
When you have create-temp_interfaces set to yes, do the interface features need to be written back the sub-component or is this always maintained within the using assembly?
Aleksey, are you referring to patterned components tied to a reference pattern when you say "repeated"?
Antonius,
If I'm interpereting "patterned components tied to a reference pattern" correctly, then no. For example, when I constrain a fastener to a patterned hole, I can press the pattern button and Creo properly places that fastener into every hole of the pattern.
What I'm talking about is the situation where I may need to put a given fastener into a few different holes on the assembly, some of which may be in independent patterns on different parts of the assembly and some of which may just be individual holes.
What I'm missing from WF5 is the fact that I used to be able to take my fastener, mate its axis to the axis of the hole it's going into and mate the underside of its head to the surface of the part that the hole is in. Then, every time I needed to place the same fastener in a different hole that did not belong to the pattern of the original hole, all I needed to do was click on the axis of the new hole and the corresponding surface and the fastener would be placed correctly.
So really, my issue is that when I try to constrain multiple instances of a given component to a few non-patterned features of the assembly, Creo does not remember the features of that component that were used to constrain it to the assembly the first time. As such, I find myself having to reselect the features of the component that I want to constrain to the assembly every single time I place a new instance of it, which is what I thought the OP's issue was. I figured there must be some default setting that has changed between the two releases, and the fix would be to simply enable it.
Hope that made some sense, and that I interpereted your reply correctly. Eagerly awaiting your reply!
I see. Yes, this very much sounds like the setting of this discussion. Maybe in WF5, it was set to yes by default and in Creo 2, it was set to no. I haven't done this so I cannot comment on the how the setting is performing.
Excellent, then that is what I will try. I'll give it a shot when I retrieve my work laptop, and report back whether it works out for me or not. Thanks for the confirmation!
Yep, fixed! Thanks, everyone!
Gotta love this forum... learn something new every day!
Aleksey, Antonius
I am a bit puzzled now.
As correctley mentioned above, this behaviour is governed by config option create_temp_interfaces = No*/Yes.
Default value of this option was No ever since it was introduced (I guess Wildfire 1 or 2), so the fact that you see changed default behaviour in Creo02 sounds fishy. Can this be you run from different start directories that have different config.pro files ?
if you run from the same place, have no config.pro and see different behaviour I'd suggest to log case to TS with models / trail file.
In general, placement with interfaces is governed by several configuration options (besides the abowe one) :
comp_assemble_with_interface ; check_interface_criteria ; check_interference_of_matches ; comp_interface_placement ; include_sub_models_interfaces. All have reasonable descriptions of what each one defines. All the same settings can be accessed already in placement dashboard in Options tab, and in Settings dialogue / Assembly Settings.
When TEMP_INTFC001 is used, there is no need to store it in part - this is a meaning of temporary interface (for those customers who have locked / released library parts like bolts / fasteners etc).
Still if you want to store this interface for future usage in another assemblies you have RMB / "Save as Interface" option while in placement process. Thsi eventually rev's the part.
Couple more tips if you come to the field of interfaces (including TEMP_INTFC) :
- you have an option to place same component several times inside single placement session - use RMB / new Location (or same in Placement tab) for this. Very fast way for placing same bolt to several holes and likevise.
- for multiple placement you have also "Auto Place" button - this one will search for suitable locations for your part basing on its interface and assembly geometry, and suggest you where it can fit in assembly.
"- you have an option to place same component several times inside single placement session - use RMB / new Location (or same in Placement tab) for this. Very fast way for placing same bolt to several holes and likevise."
no such option seen..am i missing something here?...creo 2.0 M050
oh got it..i think it works with temp_interface only..as you have mentioned..thanks
well, it should work with any interface - the only difference of TEMP_INTFC is that it is recognized on the fly from already placed component(s), not stored with the model.
Btw if your component is placed in assembly in more than one way - you will get more than one TMP_INTFC to choose from ...
never new these options existed.....i bieleve this is where PTC lacks..to give the right training...Pro/E is wonderful and very powerful software....and as when i come to know new options...the power only increases..PTC should surely share the good things...not thought about how it should be done.....but yes it should surely be done....i mean you develop the software..you know it most..then you should share it..it would only help you the most in long run....
Rohit,
I am 100% with you on this statement. We should promote better new enhancements.
Looking at the related topics, there is quite a lot info about Interfaces and placement with Interfaces - browsing Help system on this one might be useful. Though I'd agree that dedicated session (live, or by several videos) would be way more helpful. here is some frmo the help center (it covers TEMP_INTFC topic also) :
To Define a Component Interface Template
To Place a Component Using Interface Matching
To Redefine Component Placement Using Interfaces
To Save a Component Interface When Placing a Component
To Set Rules for Assembly Conditions
To Place a Component Using Interface Matching
Is the TEMP_INTFC located in the Configuration Editor or when you click on Assemble to add assembly components...or perhaps somewhere else?
- you have an option to place same component several times inside single placement session - use RMB / new Location (or same in Placement tab) for this. Very fast way for placing same bolt to several holes and likevise.
I never knew that, but it sounds like exactly what I need. Thank you! I think I've learned more browsing this forum than I ever did in the college course where we were taught to use ProE/Creo.
- for multiple placement you have also "Auto Place" button - this one will search for suitable locations for your part basing on its interface and assembly geometry, and suggest you where it can fit in assembly.
I've never had much luck with this feature, but perhaps I'm going about it wrong. Also something to look into in my spare time!
Is there a specific type of assembly file that needs to be selected to make this work? I've been picking the default 'Design' form of an assembly file, but I don't have any options for placing multiple components.